[cliffaddy]

Hey guys, total newbie here ...

I'm looking to get my first CNC mill. Right now, I'm planning to get Grizzly's version of the Super X3 and CNC it with CNCFusion's kit.

I'm going to working almost completely in 7075 aluminum. From what I've read, aluminum should be milled at far higher spindle speeds than the Grizzly's top speed of 1750 rpm, which seems to limit it to about 20 ipm.

My budget is limited, but I need to able to produce parts in a reasonable amount of time. Right now, simulations at 20 ipm are coming in at several hours. How can I improve the mill's performance? I have a 5hp motor lying around, can I simply install a bigger motor and change the gearing or will that blow out the bearings? Can I feed at at higher rate by using carbide or adding a flood coolant system?

Is there a better choice for the mill? I really can't swing more than $3500 or so for the mill, motors, and control, so I can't simply go buy some monster mill.

Any advice would be greatly appreciated.

Cliff

[SCzEngrgGroup]

You don't indicate what type of work you will be doing, and what size tooling you'll be using most. RPM is determined by tool material, tool diameter, and work material. If you'll be using 1/2" HSS tools in aluminum, you *want* to be turning about 3100 RPM, and feeding at 10-15 IPM, faster for shallow cuts. If you'll be using 1/8" HSS tools in aluminum, you *want* to be turning about 12,000 RPM, with about the same feed rates (maybe a bit less).

So, yes, 1750 RPM will SERIOUSLY increase your machining times. Except for larger tools, you don't need more power, you need more RPM. you can probably get away with perhaps doubling the RPM by changing motors (get a 3-phase motor and VFD, which will allow you to double the motors base speed, and give you variable speed), or gearing (a LOT more work). Better still, get a mill that already has higher speed capability. Syil has an X4 mill with, IIRC, a 24K RPM spindle. But, it may be vaporware.

I can't for the life of me understand why all these small mills have such low speed spindles, as it is a serious performance limiter. Of course, given their limited rigidity, you aren't likely to reach the above rates on other than very shallow cuts anyway. $3500 just doesn't buy you a very heavy duty CNC machine.....

Regards,
Ray L

[cliffaddy]

So, would I be better off going with a Taig? Their machines have a top speed of 10,000+ rpm. The parts I'm machining will all be fairly small, 12"x6"x4" max.

[Stepper Monkey]

Except for larger tools, you don't need more power, you need more RPM.


Shhhhh. Don't start in with all these newfangled ideas that use that strange "logic" stuff! You'll rile the natives. Remember the chant, "if it weighs more, it must work better".
Sheesh. Next you'll try telling us that TruckNutz don't actually add 50 extra Horsepower, or that the Earth goes around the Sun or something else equally silly.
Jeez, kids these days...

[ImanCarrot]

[quote]Remember the chant, "if it weighs more, it must work better"

lol, I like that

Gonna print that out and stick it on my lab wall.

[SCzEngrgGroup]

So, would I be better off going with a Taig? Their machines have a top speed of 10,000+ rpm. The parts I'm machining will all be fairly small, 12"x6"x4" max.

You definitely want to find a machine with the fastest spindle you can. A Taig might be a good choice - I'm not sure what it's actual usable work envelope is. I suspect the size you specify may be pushing it. The Taig is a pretty flexible machine, which means you won't be doing any heavy cutting, but you would be able to move fairly fast with small cutters. You might also look at the Syil X4. There is a model with a high-speed spindle (20K RPM, IIRC), though it's a bit outside your budget. As in most things - You can have good, cheap, fast - pick any two.

Regards,
Ray L.

[hoss2006]

Himmy can attest to the logic that a larger machine can take MUCH bigger DOC's
getting your part finished much sooner than a tiny machine that has to tickle away
even with it's higher rpm.
Do a search, someone posted a simple upgrade to the X3 to increase the rpms.
Even at only 1800 and corresponding SFM, you can see it's capable of a decent feedrate.

[Andre' B]

I can't for the life of me understand why all these small mills have such low speed spindles, as it is a serious performance limiter.

Lawyers and liability.
When selling to a commercial shop the manufacture has some protection and can reasonably assume the person operating the machine has some level of qualification. Also cost is not as big an issue as it is at the hobby level, so the manufacture can put proper shielding and safety switches on the machine to make sure the doors are closed.

Selling to the hobby market the operator could be some 14 year old kid with no experience, no guidance, and no common sense. Sooner or later someone is going to put a fly cutter in the spindle, spin it up to 30,000 and the 1/4 HSS tool bit is going to end up buried in the wall after passing thru the kids guts.

[hoss2006]

Lawyers and liability.
When selling to a commercial shop the manufacture has some protection and can reasonably assume the person operating the machine has some level of qualification. Also cost is not as big an issue as it is at the hobby level, so the manufacture can put proper shielding and safety switches on the machine to make sure the doors are closed.

Selling to the hobby market the operator could be some 14 year old kid with no experience, no guidance, and no common sense. Sooner or later someone is going to put a fly cutter in the spindle, spin it up to 30,000 and the 1/4 HSS tool bit is going to end up buried in the wall after passing thru the kids guts.

Good point!
We have signs posted on all our equipment at work forbidding usage by unauthorized personnel, with their jobs at risk if they do.
Protects them and us from machinery that could kill.
The hobby machines have to build in the protection to keep the maiming to a minimum.

[SCzEngrgGroup]

Himmy can attest to the logic that a larger machine can take MUCH bigger DOC's
getting your part finished much sooner than a tiny machine that has to tickle away
even with it's higher rpm.
Do a search, someone posted a simple upgrade to the X3 to increase the rpms.
Even at only 1800 and corresponding SFM, you can see it's capable of a decent feedrate.

A 1/4" tool running a 0.005" chipload will not live very long at all. Running a 4-flute 1/4" tool in aluminum will clog in a few seconds, unless perhaps making very shallow cuts. That 36 IPM feedrate would work only on a very shallow cut anyway, and you'll end up with a whole drawer full of endmills that are dull on the tips, an unused over most of their length. Any reasonable depth of cut on a small mill, and the vibrations will beat the tool to a pulp in very short order. The best way to get your money's worth out of tooling is to keep the RPMs and chiploads reasonable, and bury the tool as deep into the work as you can, so you're using as much of the length of the tool as possible. Slow down the feed until you're just short of breaking the tool, and/or stalling the spindle.

Regards,
Ray L.

[HackMax]

A 1/4" tool running a 0.005" chipload will not live very long at all. Running a 4-flute 1/4" tool in aluminum will clog in a few seconds, unless perhaps making very shallow cuts. That 36 IPM feedrate would work only on a very shallow cut anyway, and you'll end up with a whole drawer full of endmills that are dull on the tips, an unused over most of their length. Any reasonable depth of cut on a small mill, and the vibrations will beat the tool to a pulp in very short order. The best way to get your money's worth out of tooling is to keep the RPMs and chiploads reasonable, and bury the tool as deep into the work as you can, so you're using as much of the length of the tool as possible. Slow down the feed until you're just short of breaking the tool, and/or stalling the spindle.

Regards,
Ray L.

Dammit so I bought my X3 for nothing then since I bought it primarily for 5/8" x 5" x 10" aluminum milling? Most of my cutting will be done with a 3/16" endmill. What should I do? What's the max DOC, speed and feed I can expect from it?

Rick

[SCzEngrgGroup]

Rick,

I can only tell you what I do on my knee mill. I run 3/16" endmills at 8200 RPM, about 10-15 IPM, 0.100" DOC, with mist coolant. I haven't spent a great deal of time optimizing the DOC and feed, since I don't do a huge amount of cutting with small tools. But, I don't think I'm terribly far from the limits. With an X3, I think you're limited to 2000 RPM, so your feed would be roughly 1/4" that. You can push it harder, but tool life will suffer.

Regards,
Ray L.

[SCzEngrgGroup]

You may find this useful, from another thread a few weeks ago:

RPM is determined by tool diameter, and material, by calculating SFPM - Surface Feet Per Minute as follows:

SFPM = (PI * ToolDiameter * RPM) / 12 or,

RPM = (SFPM * 12) / (PI * ToolDiameter)

This is usually rounded to:

RPM = SFPM * 4 / ToolDiameter

SFPM is a function of the tool material and the work material. For mild steel being cut with HSS cutters, SFPM should be around 80. For aluminum, 400 SFPM is a good average. If using carbide, double or triple those numbers. So, if you're cutting mild steel with a 1/2" HSS endmill:

RPM = (80 * 4) / 0.5 = 320 / 0.5 = 640 RPM

Feed rate is a function of RPM, the number of flutes on the tool, and the "chip load", which is the nominal thickness of the chip each tooth carves out:

FEED(in IPM) = RPM * #Flutes * ChipLoad

Chipload is a function cutter diameter, and for roughing cuts ranges from perhaps 0.0004" for very small endmills (1/16") to perhaps 0.008" for large ones (1"), and varies linearly for sizes in between. So, for a 1/2" 4-flute endmill, assume a 0.004" chipload, and you get:

FEED = 640 * 4 * 0.004 = 10.2 IPM

Depth of cut should be as much as you can get away with, which will be limited by spindle power, machine rigidity, and coolant used.

Now, you're not likely to reach this numbers on a small mill, due to the limited spindle power, limited rigidity, and inadequate cooling. So, start by setting the calculated RPM, pick what you feel is reasonably modest depth of cut, and start by feeding at perhaps half the calculated rate. Increase feed rate until finish quality starts to degrade. When you reach that point, back off on the feed rate perhaps 10%. Now increase depth of cut until the machine starts shaking, or the spindle motor starts laboring, then back off a bit.

There are no canned numbers, as every job is different, and you have to learn how to "read" the machine. Some rules of thumb:

Keep chip load as high as possible. If you find you have to reduce feed rate well below the calculated value, then reduce the RPM to keep the calculated and actual feed rates reasonably close. Running high RPM with low chip load will cook tools faster than anything.

USE COOLANT!! You will never come anywhere even close to the calculated numbers without coolant. A mist system will work wonders, with very little mess.

Here are some typical numbers I use on my knee mill, running mist coolant:

1/2" 4-flute HSS endmill cutting 1018 steel: 700 RPM, 5 IPM, 1/2" DOC
1/2" 2-flute HSS endmill cutting 6061 aluminum: 3100 RPM, 12 IPM, 1/2" DOC

Regards,
Ray L.

[hoss2006]

Exactly, that was my point. A lot of RPM's aren't going to do you any good
if the machine isn't rigid enough to take advantage of them.

I found these Feed/Speed, Calcs and Charts to be a big help.
They can get you in the ballpark but experience will be your best guide.

[philbur]

I think fast spindles are good with repsect to machines that are limited in rigidity as you still get the horsepower transmission with out the high torque. It's the torque being transmitted that is the constraint when it comes to rigidity. The apparent, dynamic rigidity of the machine increases with increased rpm. I think it is the same reason why you can hand-hold a 1 horse power router but not a 1 hp cold saw.

Just a thought, I'm interested to know if my understanding is correct.
Phil

[sansbury]

Phil, that's my understanding too. All things being equal, with CNC I've learned to run the speed and feed twice as fast, but 1/2 the DOC. You remove the same amount of metal in the same amount of time, but you get a much nicer finish. I think of it as ghetto HSM.

[SCzEngrgGroup]

I think it is the same reason why you can hand-hold a 1 horse power router but not a 1 hp cold saw.
Phil

No, that's a function of torque. With a router, you have a very low-torque motor spinning at 25K RPM, turning a very small cutter. The small cutter makes a very short moment arm, so the torque you have to resist is relatively low. A cold saw spins perhaps 3600 RPM, with a 7-10" diameter blade. That same 1 HP comes from the much higher torque at the reduced RPM. The large blade makes a large moment arm, so the torque you have to resist is enormously higher.

Regards,
Ray L.

[philbur]

I thought that was my point but maybe I didn’t make myself clear. Low rpm requires a higher torque, for the same hp, than high rpm. Th reason you can handhold the 1 hp router is the lower torque.

Its torque that produces machine (or people) deflections not necessarily horsepower.

Is this the essence of dynamic stiffness?

Phil

No, that's a function of torque. With a router, you have a very low-torque motor spinning at 25K RPM, turning a very small cutter. The small cutter makes a very short moment arm, so the torque you have to resist is relatively low. A cold saw spins perhaps 3600 RPM, with a 7-10" diameter blade. That same 1 HP comes from the much higher torque at the reduced RPM. The large blade makes a large moment arm, so the torque you have to resist is enormously higher.

Regards,
Ray L.